Hello,

I am working on vortex shedding problem using SOLA method for incompressible flows. If you have SOLA method description or code, you can give details. This method was developed my "HIRT C.W,B.D. Nicholas,Romereo(1965), SOLA- A Numerical Solution of Algorithm for Transient flows". I shall be waiting for your reply.

I'm curious to know why you would want to use SOLA-VOF. There have been alot of achievements to VOF methods over the past 20 years... Its also very easy to extend the piece-wise constant method to piecewise linear...

Anyway, here are two references which might help:

Nichols, B. D., Hirt, C. W., and Hotchkiss, R. S., "SOLA-VOF: A Solution Algorithm for Transient Fluid Flow with Multiple Free Boundaries," Los Alamos Scientific Laboratory report LA-8355 (August 1980).

1981 Hirt, C. W. and Nichols, B. D., "Volume of Fluid (VOF) Method for the Dynamics of Free Boundaries," J. Comput. Phys. 39, 201(1981).

Hello,

Thanks for you reply. But, I am using SOLA only, not SOLA-VOF. The SOLA method is developed by LANL in 1975. If you have some idea over it, you can clear my doubt. I am using this method for " Flow past a square cylinder". In case of transistional reynolds number, the vortex shedding frequency what I am getting from program is not matching with the experimental results. So, I believe there will be some mistakes in implementing this code. If you have an idea, you can guide me in this matter. I shall be waiting for your reply.

The SOLA series of codes uses a donar-cell (up-winding) technique for fluxing of momentum. The parameter that controls the amount of upwinding is usually coded as "ALPHA". The range is 0.0 <= ALPHA <= 1.0.

Beyond stabilizing the calculation, upwinding introduces an artificial viscosity-like term that is proportional to ALPHA, the time step, and the absolute value of the local flow velocity. This 'computational viscosity' means that the Reynolds number of your calculation is different from that of the flow you're trying to simulate. In this case, your calculation will produce a shedding frequency that matches the Reynolds number calculated using the sum of the physical and artifical viscosities, NOT for the physical flow specified in your input.

You might try a smaller ALPHA and/or a smaller time step. These are related through the various stability rules given in the LASL reports cited previously.

Good luck!

Hello,

I have done as you said. I have taken alpha as 0.2 and time step as 0.002. delx as 0.2 and delt as 0.125 and re as 140. But, the strouhal numbers are not matching with experimental values eventhough, we consider the computational viscosity. I shall be waiting for your kind reply.

The errors generated by the donar-cell differencing are detailed (along with the method for calculating them) in

C. W. Hirt, "Heuristic Stability Theory for Finite-Difference Equations", J. Comp. Phys., v. 2, p. 339 (1968).

Another possible source of error is lack of resolution of the flow over the obstacle used to generate the vortices. You may want to experiment with the BC specified on those surfaces: Free slip or no slip? Especially if you're using no slip, resolution of the resulting boundary layers should be investigated.

Hope this helps.

> Especially if you're using no slip, resolution of the resulting boundary layers should be investigated.

If he uses free slip, he will see NO vortex shedding. He'd have to use no-slip of course.

When you say your Strouhal number doesn't match that of the experiment, you're only telling half the story, really. You need to be more specific. What is the number you get and what is the experimental value? AND what is the error bar for the experiment? Are you out of this range? If so, then you have to make sure that the experiment is accurate (check out other experiments). Once you've completed your preliminary homework, then you'll have to start working on the numerical end of things.

For example, how far out is your outer domain (and how close is it to the experimental setup)? The "blockage" affects flow physics dramatically. Note, even if you specify free-slip velocity at the outer edges the square cylinder will still feel the effect of the outer boundary if the latter is not far enough. And of course you have to make sure that you are resolving the boundary layer as recommended earlier. Note, you are looking at the physics of (unsteady) vortex "shedding", then you'd better be capturing the (unsteady) generation and shedding of vorticity accurately. This means that you need to resolve not only the "traditional" boundary layer but a larger area outside it, because the boundary layer is unsteady.

Adrin Gharakhani

"If he uses free slip, he will see NO vortex shedding. He'd have to use no-slip of course."

I wonder about this. If the questioner were doing flow over a cylinder, the classic vortex-shedding configuration, I would absolutely agree. In that case, the boundary layer is forced into separation when the Reynolds number lies within a particular range. The separation is forced by the adverse pressure gradient on the back slope of the cylinder.

But the questioner is asking about flow along the surface of a square obstacle (see the third post in this series). The separation occurs at the back corner of the blockage. Seems likely that the energetic flow past the block would not make the right-angle turn even with some retardation due to a boundary layer. And, if it doesn't make the turn (that is, it separates!), a vortex is generated by flow induced along the back face. In other words, free-slip or no-slip over a square block might modify the details, but shedding would occur within the appropriate range of Reynolds numbers in either case.

There's a relatively simple computational case that could take the boundary layer out of the picture (Thanks to Dr. Larry Cloutman of the Lawrence Livermore National Lab for suggesting this). Specify constant inlet velocity on one face of a region except for a few no-flow cells that mimic the back face of the obstacle (the obstacle is upstream of the flow). Does the computed flow generate a vortex street in the appropriate range of Reynolds number?

This is of course all an aside to the original question. To the student: Once again, good luck with your project!

(1). I have not followed this thread closely, but, I think, Adrin is right. (2). The flow separation on a surface is a viscous effect. (forget about other possible causes such as a shock wave, etc.) Thus, one needs to use NON-SLIP condition on the wall. (3). I am open minded, so, I think, I can listen to your side of the story.

> The separation occurs at the back corner of the blockage

If separation occurs, even if it is due to "geometric singularity", it is because of no-slip! If you make all walls free-slip and solve the inviscid flow problem, you'll end up solving the potential flow problem (to the best of my knowledge). In this case the streamlines will follow the shape of the geometry. There will be no mechanism for flow reversal/separation/etc.

IF you get vortex shedding of sorts or separation in a backward/forward facing problem I can see two possible reasons for this to happen:

1) You are using a numerically viscous method that extends to the boundary,

2) You are "modeling" separation at the "geometric singularity". But the model implicitly assumes viscous action.

> a vortex is generated by flow induced along the back face

Though there is controversy regarding the exact mechanism for vorticity generation on the wall (and some famous professors - unfortunately - have even argued that you can have inviscid vorticity generation), vorticity is generated on the walls due to viscous effects.

Indeed, if you were using a vortex-based methodology to solve this problem it would become immediately obvious that vorticity is generated to satisfy the no-slip boundary condition - just as in nature!

To give an example, based on personal experience, if you try to simulate flow in an engine and assign free-slip on the valves, guess what happens to the flow in the engine chamber. The primary eddy rotates in the opposite (physically incorrect) direction! This is because near the valve the streamlines are following the geometry shape and go under the valve (instead of "separating" at the valve) and begin to rotate in the wrong direction. The reason there is any rotation in this example is because all other walls are assigned the no-slip BC. Otherwise, if all walls were assigned free-slip BC, there would be no eddies to rotate in the right or wrong direction!

Adrin Gharakhani